Hello Richard,

I find it helps to make a one element model to understand what material models are doing. I made a 10 mm cube and meshed it with one linear element so there are only 8 nodes. I used symmetry on each of the three adjacent faces to hold the cube, then I applied a 0.02 mm displacement on the face normal to the X axis.

I created a simple material with E = 100 GPa and used Bilinear Isotropic Hardening with a Yield Strength of 100 MPa and a Tangent Modulus of 0.

All these plots are vs. Time, so at 1 the displacement is 0.02 mm on a 10 mm cube or a total strain of 2.e-3 as shown in the plot below.

You know that Total Strain = Elastic Strain + Plastic Strain. In the plot of elastic strain, you can see that at a strain level of 1e-3 (time = 0.5), the elastic strain reaches the point when plastic strain begin. This is expected because Yield Strength/Modulus = 100 MPa / 100 GPa = 1e-3.

Plastic strain is zero below the yield stress and then it increases.

The stress increases until it reaches the yield stress.

If I plot Normal Stress (Max) vs. Equivalent Total Strain (Max) I get the material Stress-Strain curve.

Hope this helps. ANSYS 2019 R3 archive is attached.